CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Mesh Refinement vs Residual/Convergence in Turbulence

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 22, 2019, 08:57
Default Mesh Refinement vs Residual/Convergence in Turbulence
  #1
New Member
 
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8
JoshuaB is on a distinguished road
I was hoping someone can help me get insight into the issue of mesh-refinement vs. convergence issues.

Firstly my setup:
I have a cylinder inside a cylinder. The outer tube has two openings 180 apart from each other. The flow enters and leaves through these holes. The flow is thus forced to go around the inner cylinder. But due to the outer cylinder the flow is fairly confined and there is a quite a bit of wall effect. I am in the turbulent regime, and hence due to the large amount of wall effect I chose the SST turbulent model. I am running this as a RANS Steady State.

I ran the solution at various flow rates. Convergence was good. But I wasn't sure if the solution was accurate, that is if my solution was mesh independent. So I decided to refine the mesh. I basically created a mesh with 4x the number of elements.

At high velocity flows the convergence is a lot worse. But the value of interest (pressure loss across the flow path) also changed quite a bit (about 15 to 20% different).

And before anyone asks, I tried running with double precision, but no change was observed in the residual levels.

The high residuals occur on the far side of the inner cylinder where the flow around the cylinder converges back together.

My working assumption is that I have refined too far and I am now picking up some of the larger scale eddies. But now I am stuck with a conundrum.

1) The change in mesh size seems to indicate that the mesh wasn't refined enough for high flow rates (in that the value of interest significantly changed).
2) The change in mesh size seems to be have picked up some of the larger scale eddies, preventing the residuals from going to a decent level for convergence.

So is the only way I can now tell at high flow rates if my mesh resolution was sufficient would be for me to run the solution as transient?

Any insights would be appreciated.
JoshuaB is offline   Reply With Quote

Old   February 22, 2019, 10:31
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,266
Rep Power: 24
Opaque will become famous soon enough
What happens if you change the timestep?

Say increase it (which can make it unstable or converge bette), or decrease it (which may relax it a bit more)
Opaque is offline   Reply With Quote

Old   February 22, 2019, 10:48
Default
  #3
New Member
 
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8
JoshuaB is on a distinguished road
Quote:
Originally Posted by Opaque View Post
What happens if you change the timestep?

Say increase it (which can make it unstable or converge bette), or decrease it (which may relax it a bit more)
From what I understand, in CFX, in a Steady State solution increasing the timestep can have the affect of numerically diffusing the physics across more cells. Thus creating a smoother answer. Perhaps even lowering the residuals. In this case even increasing the time step by 20x did not help in any great way.

However when thinking about it, wouldn't increasing the pseudo time step work against the reason I made a finer mesh. My logic is that isn't the code now so to speak numerically diffusing the results from one cell over additional cells.

As for lowering the time step. That may lower the standard residuals, but I would think for the pressure differential I am looking for it would just simply slow down the peaks and valleys I see in the steady state solution, but not alter them.

If you feel I am misinformed about one or both of these issues, I would be happy to hear your logic.

Last edited by JoshuaB; February 22, 2019 at 11:10. Reason: clarity
JoshuaB is offline   Reply With Quote

Old   February 22, 2019, 11:45
Default
  #4
Senior Member
 
Join Date: Jun 2009
Posts: 1,266
Rep Power: 24
Opaque will become famous soon enough
For steady-state cases, the value of the timestep has absolutely no influence on the results if the simulation is converged. Any dependence on the timestep is a defect and a bogus solution.

However, the timestep size has a very strong influence on how fast/slow the solution converges, or if it converges at all.

Summary: timestep value is your knob to guide convergence, and it sure is related to some physics, but the final results do not depend on it.
Opaque is offline   Reply With Quote

Old   February 22, 2019, 13:28
Default
  #5
New Member
 
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8
JoshuaB is on a distinguished road
Thanks. So I guess in order to see if a steady state solution exists I need to try both increasing and decreasing the time step.

I think I understand the the decreasing the time step. My thought is that decreasing the pseudo-time step to try is analogous in Pressure based solvers of lowering the relaxation factors. So I see how this makes sense. If their is a converged steady state solution this is one way to ferret it out.

However I'm a bit more confused why increasing the pseudo time-step should work just as well. I can see how it would make things less stable, once again, similar to the making the relaxation factors too large. I'm just not sure how it can make the solution converge better. If you can help me with a justification for this I would appreciate it.

But at any rate, if these methods don't increase the solutions ability to converge, then I take it the solution is probably inherently unsteady.
JoshuaB is offline   Reply With Quote

Old   February 22, 2019, 16:04
Default
  #6
Senior Member
 
Join Date: Jun 2009
Posts: 1,266
Rep Power: 24
Opaque will become famous soon enough
Recall the use of a "false timestep" approach is trying to approximate a transient solution (all the physics in sync among all equations).

A very small timestep would approach a transient solution; however, ANSYS CFX also introduces other relaxation factors which prevent it from being a true transient. As you decrease the timestep size, the iterative process may capture some features (similar to a true transient), and those features can prevent convergence or increase the number of iterations to steady state convergence.

As you increase the timestep, you may overcome those; however, at the risk of making it unstable. That is, there may be "sweet spot" .
Opaque is offline   Reply With Quote

Old   February 23, 2019, 03:37
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
My 2c worth:

Quote:
I basically created a mesh with 4x the number of elements.

At high velocity flows the convergence is a lot worse.
This is normal. Finer meshes have lower numerical diffusion so the simulation is harder to converge. It is correct that the mesh can now resolve small flow features which were damped out on the coarser mesh, but it is also a purely numerical effect.

Increasing the pseudo time step size in a steady state simulation which is not converging well is trying stabilise the small flow features which are likely moving around (ie transient). If the pseudo time step is too large to resolve these flow features then they are smoothed out and a steady state flow field is achieved. Well, that is the theory anyway. It does not always work but is definitely worth a try.

But your comment that your mesh refinement requires a transient simulation for convergence is correct. If you cannot obtain convergence by adjusting the pseudo time step size as Opaque suggests then you have to do it transient.

But before you do, don't forget that the convergence criteria is also a parameter you should do a sensitivity study on. If you find you don't need to converge as tightly as you currently do then you might avoid this whole problem of convergence on fine meshes as a looser convergence could be OK.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   February 25, 2019, 08:31
Default
  #8
New Member
 
Joshua Brickel
Join Date: Nov 2013
Posts: 25
Rep Power: 8
JoshuaB is on a distinguished road
So if I understand you and "Opaque" correctly, refining the mesh and increasing the time pseudo-timestep will not work against each other. That is the mesh will solve with the accuracy of a refined mesh. Just some of the small scale affects which are transient in nature (and unimportant in the steady state solution) are being numerically diffused out.

The reason I created this refined mesh was to see if I was truly mesh converged (which I was not at the larger mesh). So this purpose will not be affected by increasing the psuedo-time step.

However if even in increasing and decreasing the time step my residuals, and more importantly, my variables of interest continue to bounce around at too high a level, then at that point I do need to perform a transient solution.

Would you say this is an accurate understanding?
JoshuaB is offline   Reply With Quote

Old   February 25, 2019, 19:16
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,349
Rep Power: 126
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, that sounds correct.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Tags
convergence, mesh refinement study, turbulence

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 37 July 20, 2020 05:38
[snappyHexMesh] SnappyHexMesh running killed! Mark JIN OpenFOAM Meshing & Mesh Conversion 3 March 12, 2020 17:50
[snappyHexMesh] problems generating clean mesh Christian_tt OpenFOAM Meshing & Mesh Conversion 2 June 20, 2019 05:39
[snappyHexMesh] Creating very fine, high accuracy mesh with snappyHexMesh JD_Welch OpenFOAM Meshing & Mesh Conversion 9 November 17, 2017 00:46
[snappyHexMesh] Removing further cells after SHM zonda OpenFOAM Meshing & Mesh Conversion 14 September 15, 2017 07:50


All times are GMT -4. The time now is 15:16.